Dimensioning standard for sheet metal part 3

[cinnamongirl]

I was given several sheet metal parts, they are basically U-shaped with three flat sides. I know the standard is to dimension the outside of the part along with the inside radii. However on the sketches I was given, the inside width of the U is specified, possibly because the inside surfaces will mate with another part.

What would be the appropriate way to dimension this part? Dimension the inside of the U and assign it as an inspection dimension (with an oblong box around it)? And if I do use an inspection dimension, do I still dimension the outside?

Thank you.

 

[berkshire]

If the inside dimension is a controlled dimension , if you have to dimension the outside do it as a reference dimension only.
B.E.

You are judged not by what you know, but by what you can do.

 

[MikeHalloran]

From a functional standpoint, it makes no sense to dimension the outside, since the inside is all you care about.



Mike Halloran
Pembroke Pines, FL, USA

 

[drawoh]

cinnamongirl,

Dimension whatever matters to you. In this case, it is the inside width. Don't forget to apply a tolerance no tighter than [±].015" ([±]0.4mm). Sheet metal bending is not an accurate process.

The oblong box is something SolidWorks added. It is not part of any standard I am aware of.

--
JHG

 

[3DDave]

You may also wish to add a restraint note that allows a certain amount of force to deform the part, much like would be accepted by the assembler.

 

[KENAT]

cinnamon girl, probably reiterating what others say but...

"I know the standard is to dimension the outside of the part along with the inside radii"

- That is not a standard or even common practice I'm familiar with. Generally the preference from a manufacturing point of view is to dimension to the inside since then you don't have as many compounding tolerances i.e. you don't have the additional tolerance of material thickness coming into it. However, push comes to shove functional requirements take precedence in the dimension scheme on the Engineering drawing - just remember the potential impact on cost of tighter effective tolerances. Dimensioning the internal bend radii is common practice, but even then consider if use of max dimension makes sense unless you're concerned about cracking.

"What would be the appropriate way to dimension this part?"

- As mentioned dimension it it a way that reflects end function, doing what you can to minimize tolerance build up issues etc. that can lead to needing tighter tolerances than the process readily supports.

"Dimension the inside of the U and assign it as an inspection dimension (with an oblong box around it)? "

- Unless you have some internal business standard that defines it the 'oblong' does not denote an inspection dimension per any standard I'm familiar with. Additionally I can't think of a drawing standard that really supports inspection dimensions being denoted on the Engineering drawing. Just because CAD can do something doesn't mean you should.+

And if I do use an inspection dimension, do I still dimension the outside?

Hopefully we've given enough input that this is no longer a relevant question. All I'll add is that duplicate dimensions should be avoided - I'd even think twice about adding reference dimensions unless they are really helpful.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[CheckerHater]

Let me begin with saying that there is no dedicated standard for dimensioning sheet metal parts.

You may often have to rely on "Industry standards" and "accepted practices"( found in places like

http://www.makeitmetal.com/resources/DG.asp

), which very often will contradict each other, so use your own good judgement and common sense.

Steel fabricators familiar with the manufacturing process usually have no problem dimensioning to outside of the part. In fact, they actually recommend it to their customers:

http://files.engineering.com/getfil...0-8139-4bf2-9a95-71d6d6d268fe&file=ShtMtl.pdf

Engineers less familiar with the shop practices prefer to dimension to "inside" hoping to reduce the error associated with material thickness and bend allowance:

http://files.engineering.com/getfile.aspx?folder=27a43033-a0b5-41ec-956f-e4380718cd06&file=No_2.PNG

Engineers with more experience consider both ways acceptable:

http://files.engineering.com/getfile.aspx?folder=0858c099-60b2-4fde-9400-77c9d9bca6b8&file=No_3.PNG

So, use your best judgement: If you have fit condition, that is, one parts goes into the other, dimension one of them on the inside and the other on the outside, just like you would do with the pin and hole.

Good luck!

 

[cinnamongirl]

I found a great resource online.

http://www.qualitytool.com/resources/Design-Handbook-Rev3.pdf

And the answer to my original question can be found on the second page.

"Critical Dimensions Sheet Metal Forming – Outside dimension should be used unless the inside dimension is critical."

 

[JNieman]

@drawoh:

I wanted to comment on your comment about tolerances on sheet metal parts. I a similar statement in these boards several times recently, it seems, and it appears to have triggered me into posting - must be a pet peeve of mine.

Just because it's a sheet metal part, doesn't mean you can't dimension it with a tolerance tighter than +/- .015" If the part requires a tighter tolerance, it requires a tighter tolerance. The _design_ either does, or does not, require a certain level of tolerance. If the design can allow +/- .020" then why was it ever tighter than that in the first place? Why would "oh it's a sheet metal part" be deciding the design allowance?

If the design requires a tighter tolerance, then maybe post-forming processes are required. Or maybe you form that flange first, and everything else afterward, with more leeway.

I know I may be picking nits, and I don't mean to focus on you specifically drawoh it's a culmination of multiple posts I've seen with a similar sentiment.

 

[CheckerHater]

@JNieman;

You are absolutely correct. You can put absolutely any tolerances on your drawings. However, as D&T expert you probably promised your employer that "correct" or "proper" tolerancing will save money.

This is exactly the reason why sheet metal fabricators (and some time educators) are publishing tolerances that are achievable at reasonable cost.
Examples can be found here:

http://www.vista-industrial.com/sheet-metal-tolerances.php#3

here:

http://www.scandic.com/images/formed-parts-tolerances.pdf

here:

http://web.mit.edu/2.75/resources/random/Sheet metal Tolerance 2.pdf

and in some other places you can find.

Because if the design requires a tighter tolerance, maybe sometimes it's better not to make it from sheet metal.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[JNieman]

I mostly agree and to discuss further would only apply to specific "in this case" and "well not if..." situations. On the large though, my only gripe was the thought process. "This is a sheet metal part, so make the tolerances no less than..." rather than "The tolerances must be +/- .003in so is there a better way to make this part?"

Plus, if you have a good supplier (cares about quality) with good machinery (CNC brake press) and the design of the part accommodates it, you can get better than +/- .015 right off the press. This is where we depart from rules-of-thumb, though, obviously.

Regardless, yes, my point was more about ensuring we're putting the horse before the cart, rather than the other way around.

 

[CheckerHater]

@ JNieman: Let me agree one more time.

It just I have pet peeve of mine too - overuse of "functional" to the extent of becoming marketing rather than technical term.

As we design part that will function, let's not forget that manufacturing process is the reason we have tolerances.

"For every expert there is an equal and opposite expert"
Arthur C. Clarke Profiles of the future

 

[drawoh]

JNieman,

As noted above, [±].015" is what sheet metal shops can do, cheaply. If you place [±].015" and [±].030" tolerances all over your drawing and one additional dimension at [±].010", the shop knows which dimension is critical and difficult. Your reasonable tolerances everywhere else shows that you are serious about the tight one. Fabricators are accustomed to idiots specifying sheet metal and weldment tolerances at [±].005".

Otherwise, if [±].015" does not work for you, you need some other method of fabrication.

--
JHG

 

[DiegoLGraves]

For what it's worth, my work is primarily sheet metal fabrication, anything from small light weight brackets to store displays to large heavy fabrications used in construction and military vehicles. For highly engineered fabricating we quote to the customer's tolerances or request deviation approval. If we can't find a method to ensure requirements are met we no-quote.
For almost all others we quote to our general process capabilities:
LASER/PUNCH LOCATION TOLERANCE ±.015
LASER/PUNCH HOLE SIZE ±.010; PEM HOLES PER STANDARD
FORMING TOLERANCE ±.030, ±1°
SAWING TOLERANCE ±.030, ±1°
WELDING COMPONENT LOCATION TOLERANCE ±.06
WELD SIZE EQUALS THE THICKNESS OF THE THINNER MATERIAL

We don't use the customer prints in our shop or for our subcontractors, and tolerances on our prints reflect the process capabilities but also controls the item requirements. Often we get an entire project group of parts so we can see the fit-up relationships that need to be held. Where ever possible we suggest changes to parts to keep costs down and ensure fit-up, such as changing clearance holes to slots. This helps keep us competitive.

All that said, with the modern accurate machines available in many fab shops today, controlling tight tolerances of less than 0.15 is no big deal. When I started work almost 40 years ago in fabricating many of our customers at the time were in aerospace, electronics, and military. Tolerances on many parts were ±.005 on formed parts made with non-cnc controlled machines (have you ever worked a kick_press?). We knew what was expected and learned to work to those tolerances without excessive behavior needed.

 

[SeasonLee]

@cinnamongirl

Example 1 and 2 in page 19, they are all inside dimensions.The figure in Page 32 use inside dimension as well.
Please ref this red book from Dayton Rogers, they are professional stamper for 3 generations.

Season